.5" Acrylic speeds?

This forum is for general discussion regarding VCarve Pro
snapajap
Posts: 13
Joined: Sat Nov 26, 2016 6:44 pm
Model of CNC Machine: Shapeoko3

.5" Acrylic speeds?

Post by snapajap »

I have read a lot of discussions about acrylic speeds and I am left scratching my head. I have had success and failure in this and I can't figure out where I went wrong. I am using a Laguna Swift table and spindle. I am cutting black acrylic (cast I think?), it seems hard and loud when cut. I last cut a rebate (pocket) of 8mm and had mini chips along the finished edge. I'd love to get some good feedback about ipm and rpm etc.
Thanks for any help, I'm a newbie, so go easy :)

ger21
Vectric Wizard
Posts: 1592
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Lake St Clair, MI, USA
Contact:

Re: .5" Acrylic speeds?

Post by ger21 »

What bit are you using?
Gerry - http://www.thecncwoodworker.com

User avatar
Xxray
Vectric Wizard
Posts: 2300
Joined: Thu Feb 17, 2011 8:47 am
Model of CNC Machine: CAMaster Stinger 1
Location: MI USA

Re: .5" Acrylic speeds?

Post by Xxray »

Generally, you want to use low rpm's and high feed rates with acrylic to minimize melting issues. Good sharp bit probably most important factor of all.
Also, freezing temps that many of us are going through is a factor, makes acrylic more brittle and prone to fracturing.
Doug

snapajap
Posts: 13
Joined: Sat Nov 26, 2016 6:44 pm
Model of CNC Machine: Shapeoko3

Re: .5" Acrylic speeds?

Post by snapajap »

First off, thanks very much for taking the time to respond!!!

The bit I have been using (and reading I shouldn't) is a 4 flute up cut 3.75 d. I'm in Los Angeles, it's been "cold" here lately, but not cold cold. So I ordered a O flute (what ever that is?) and that should be tomorrow. I think I ran at 18,000 rpm and 75ipm, I've since read that's backwards. I was doing 2.5mm passes too..It was loud and slow and poor quality.

mark-s
Vectric Craftsman
Posts: 216
Joined: Sat Feb 03, 2018 2:03 am
Model of CNC Machine: diy 4 X 4 CNC Router
Location: So. Cal.

Re: .5" Acrylic speeds?

Post by mark-s »

With a zero flute,6 mm bit, I run at 13000 rpm seems to work good.
mark-s

snapajap
Posts: 13
Joined: Sat Nov 26, 2016 6:44 pm
Model of CNC Machine: Shapeoko3

Re: .5" Acrylic speeds?

Post by snapajap »

Thanks Mark!

I meant to say I was using a .375" bit, so like 9.5mm. Sorry.

snapajap
Posts: 13
Joined: Sat Nov 26, 2016 6:44 pm
Model of CNC Machine: Shapeoko3

Re: .5" Acrylic speeds?

Post by snapajap »

Mark, what feed rate do you use?

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: .5" Acrylic speeds?

Post by martin54 »

Acrylic is not as forgiving as wood so making sure your speed & feed settings are correct is much more critical, cast acrylic will machine better than extruded & there is very little difference in cost these days. Correct speed & feed settings will vary from machine to machine so what works well for one person often won't work well for another. You are really best running your own tests, you have a machine that is not very ridged, don't know what machine Mark has but his settings may be totally unsuitable for your set up.
As well as the correct settings & a sharp bit chip extraction is very important to prevent recutting & welding of the cut chips, if your extraction system isn't great then an airline blowing on the cutting area will help, not only keeps the cutting area clear of cut chips but also helps to cool the cutter. Doesn't need to be much just a gentle blow is enough.
I wouldn't use 4 flute bits for anything with a hobby type cnc router, you will never match speed & feed settings for any type of material unless you are running a low speed spindle, single or 2 flute cutters are what you should really be looking at buying for your machine :lol: :lol:

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: .5" Acrylic speeds?

Post by Leo »

You should NOT use a 4 flute cutter.

Also the ratio between your EXTREMELY high RPM and very low feedrate together the 4 flute cutter is a horrible combination.

On soft materials use as few as possible flutes. One or two flutes is best. Some special cutters are 3 flutes but this is a max on flutes in soft materials

4 flutes in a cutter is for steel.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

snapajap
Posts: 13
Joined: Sat Nov 26, 2016 6:44 pm
Model of CNC Machine: Shapeoko3

Re: .5" Acrylic speeds?

Post by snapajap »

Thanks all so much! I'll be slowing the rpm, speeding up the feed and reducing the flutes. I'll do a few test runs today and post some results.
Thanks every one, what a great forum this is!

snapajap
Posts: 13
Joined: Sat Nov 26, 2016 6:44 pm
Model of CNC Machine: Shapeoko3

Re: .5" Acrylic speeds?

Post by snapajap »

Soooo....

It seems I am cutting 1/2" cast acrylic. The edges are ever so slightly chipped. I used a 2 flute bit and slowed the rpms down to 7k, feed rate of 70ipm and quite a clean finish but not perfect. I actually got better results from the 4 flute bit, but still not perfect. Any ideas?

Thanks!!

User avatar
Xxray
Vectric Wizard
Posts: 2300
Joined: Thu Feb 17, 2011 8:47 am
Model of CNC Machine: CAMaster Stinger 1
Location: MI USA

Re: .5" Acrylic speeds?

Post by Xxray »

Chipped edge are indicative of:
* Too high speeds
* Dull bit/sub optimal bit
* Machine flex
* Improper holddown
Or any combination of those, and one could cause the other.
Might be best to get it as good as you can and buff out the minor flaws, tough for the average DIY'er to get consistent perfection with plexi. Edges almost always need some work in the best of circumstances. If you plan on working with plexi alot, you'll need to invest in a good buffer, expecting flawless pieces off the table is asking too much.
Doug

snapajap
Posts: 13
Joined: Sat Nov 26, 2016 6:44 pm
Model of CNC Machine: Shapeoko3

Re: .5" Acrylic speeds?

Post by snapajap »

That was a great response Xxray! Thank you

User avatar
Xxray
Vectric Wizard
Posts: 2300
Joined: Thu Feb 17, 2011 8:47 am
Model of CNC Machine: CAMaster Stinger 1
Location: MI USA

Re: .5" Acrylic speeds?

Post by Xxray »

No need to go overboard investing, I'm into plexi alot so I invested in a pro grade Baldor buffer years ago after much frustration [about $600], I can get rough edges looking like glass in minutes. But if you are already getting decent edges you might need nothing more than a mouse/orbital sander, 120 grit pads and a small propane flamer to get pro looking results.
Doug

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: .5" Acrylic speeds?

Post by martin54 »

Just to add to what Xxray has said here are a couple of other things to consider. You are using a cheap hobby machine (cheap in CNC terms) which means it has a lot of limitations. Doesn't mean you can't achieve good results but does mean you might have to work a bit harder to achieve them, obtaining perfect results may be beyond the machines capabilities. If your machine has its own forum ask questions like this on there as well as here, people on this forum are very helpful but use lots of different types of machine so what works well for one person won't always work well with your set up.

Try a single flute bit that is specifically designed for cutting acrylic, they are more expensive but will give a better finish, bits I use are from a UK Company but I believe the Osrund "O" flute bit is what people over the pond use a lot :lol: :lol: Keep that bit for cutting acrylic only & don't be tempted to use it for cutting anything else. Run a series of test cuts with varying speed & feed settings to determine the best settings for your set up, take some time with this & fine tune it to give the best results. Make sure you keep the cutting area clear of cut chips to prevent recutting, much more important with acrylic than it is with wood.

Always expect to have to do some finishing work once it comes off the machine, unlikely you will ever get a clear gloss finish off the machine, you can achieve a clean frosted look which I actually like & use quite a lot :lol: :lol:

Oh & double check what material you are cutting, big difference in cutting acrylic & polycarbonate :lol: :lol:

Post Reply